# Pressure-time plot at outlet

 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 17, 2012, 08:02 Pressure-time plot at outlet #1 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Hi there, I am a new Ansys CFX user. I have learned in the previous posts here how to have a pressure-time plot at a specific point. However, I could not find how to see pressure variation vs time at a boundary like outlet. Can you help me please? I am asked to plot p-t in outlet. I don't know what this kind of investigation tries to tell me!!

 August 17, 2012, 08:40 #2 Senior Member   Lance Join Date: Mar 2009 Posts: 606 Rep Power: 14 What about plotting: areaave(Pressure)@Outlet ? there should be an example on how to plot expressions in the tutorials.

 August 17, 2012, 09:38 #3 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Yes, I've tried so and got some results. But I wonder how one can figure out if the results are fine according to such a plot? or what does this plot really want to say?!

 August 17, 2012, 10:06 #4 Senior Member   Lance Join Date: Mar 2009 Posts: 606 Rep Power: 14 The plot represents - maybe not surprisingly - the average pressure on the outlet. Only you can decide what it means or if it "fine" or not, especially since you haven't told us what you are modeling...

 August 17, 2012, 10:07 #5 Member     Felipe Gobbi Join Date: Apr 2012 Location: Brazil Posts: 76 Rep Power: 7 You'll have to know what to expect from the situation you're modeling, like a pressure drop/increase to see if the results match the expected. If you plot areaAve(Pressure)@Outlet over time you'll see how the pressure averaged by the area is changing as time goes by in a transient case of course.

 August 20, 2012, 03:18 #6 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Thanks guys for your reply. The whole idea for me is how can a p-t plot a kind of evaluate my results? I am trying to figure out the amount of leakage in a flushing system. I have one inlet, and 2 outlets(One desired and one leakage). The flow is for sure a result of pressure drop. Two seperate simulations for two different fluid material : air and water are peformed. For air with steady simulation, the results while monitoring in the solver manager seems quite nicely converged. But for water (steady simlulation), some oscillations appear while monitoring the results. However, I see small changes in U-mom, V-mom, W-mom and P-mass in the output file. Still, I decided to do a transient simulation to probably see smoother results, but bigger wiggles appear. Now, I wonder how can I recognize if the results are real, fine or whatever!

 August 20, 2012, 06:03 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,457 Rep Power: 104 This FAQ is titled "Why is my simulation inaccurate" - but it can be looked at another way - for an accurate simulation you need to have considered these things. Have you considered all these issues? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

 August 20, 2012, 06:33 #8 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Dear Glenn, Yes, I have read it before, and I did some sensitivity analysis, but I will go through it once more, probably I get more. I know it needs experience to understand which parameters effect for example this result, so changing them can have major effects. But for me now, I did some changes, like bc, turbulence model, time step, ..., but in my point of view no specific changes happened. I read some thing about error analysis, but I think I need more detailed discriptions, any source to study? Thanks, Soolmaz

 August 20, 2012, 06:43 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,457 Rep Power: 104 The following FAQ - "Are my results publishable?" describes a very useful set of procedures to determine the accuracy of a simulation. The key text book in the field of CFD accuracy is "Computational Fluid Dynamics" by Roache.

 August 20, 2012, 06:47 #10 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Thanks for your guide. Still, I wonder what I can figure out from a p-t plot to evaluate my results? Can you please help me with this one also?

 August 20, 2012, 06:48 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,457 Rep Power: 104 If you post a description of what you are modelling, the CCL, maybe the output file and some of your results we might be able to comment.

August 20, 2012, 08:59
#12
New Member

Soolmaz
Join Date: Aug 2012
Location: Sweden
Posts: 19
Rep Power: 6
Dear Glenn,
I am trying to model a flushing system and the aim is to understand the amount of leakage from the sealing.

The required docs. including the geometry, output and result file is attached.

p.s. The result from solver manager is cut. I used some former simulation as ic for current simulation and I did not want to make it quite a mess to see!
Attached Images
 Fluid Flow CFX.jpg (27.1 KB, 14 views) run.png (8.1 KB, 11 views)
Attached Files
 Fluid Flow CFX_027.txt - Notepad.pdf (87.1 KB, 10 views)

 August 20, 2012, 10:46 #13 Senior Member   Lance Join Date: Mar 2009 Posts: 606 Rep Power: 14 So you have pressure boundary conditions on your outlets (16 Bar and 0 Pa) And you want to study the pressure on the outlets? That doesnt really make any sense. Why would the pressure change with time on your boundaries, if you prescribe them?

 August 20, 2012, 19:24 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,457 Rep Power: 104 Lance's point is important, you need to have a think about what you are trying to do with this simulation. Also your image shows the outlet at a location where I would expect lots of separations and recirculations occuring. This is a bad place to put an outlet and you will never get good convergence. You will need to move your outlet boundary down stream. Also, I can only see 1 outlet, but your CCL says there are 2, and they have massively different pressures. Where are both the outlets?

August 21, 2012, 03:29
#15
New Member

Soolmaz
Join Date: Aug 2012
Location: Sweden
Posts: 19
Rep Power: 6
Dear Lance,
First, I should mention that the results that I've just showed are steady state solution.

You are quite right but while I go to transient simulation I can see pressure changes with time for a point. Can't it happen? Because I think total pressure is constant, not the pressure in each point while time passes. Am I wrong?

Dear Glenn,
In case of recirculation at the outlet, you are quite right. Because of this, I decided to consider both outlets as openings. Probably I need to move the outlets also.

The geometry from back which shows both outlets are attached here. The reason is that, one oulet (with the bigger diameter) is where the leakage happens and this goes to atmosphere.
The other one with a smaller diamater is where the desirable flow passes.
Attached Images
 Fluid Flow CFX.jpg (26.1 KB, 4 views)

 August 21, 2012, 20:47 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,457 Rep Power: 104 Your convergence will improve a lot if you extend your domain further downstream to a location where the flow is simpler (ie no recirculations).

 August 22, 2012, 07:40 #17 New Member   Soolmaz Join Date: Aug 2012 Location: Sweden Posts: 19 Rep Power: 6 Dear Glenn I will try it also Dear Lance The thing that I finally recognized with the help of a colleague is that the pressure fluctuation vs time @oulet can show me the unsteadiness of my flow at the location of outlet. Then if I compare these fluctuations deviation from my mean pressure (of transient simulation for sure!) with the residual of my steady simulation, I can recognize if my steady solution is fine. Guys, please correct me if it is not correct.

 August 22, 2012, 08:46 #18 Senior Member   Lance Join Date: Mar 2009 Posts: 606 Rep Power: 14 Well, the "opening pressure and direction" option on an opening mean that the pressure is the total pressure when the flow is going into the domain, while it is just a relative static pressure when the flow is leaving the domain. I dont see how the pressure at outlets with recirculation will help you determine if your steady state simulation is ok?

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Artex85 OpenFOAM Running, Solving & CFD 11 February 16, 2017 14:40 a.lynchy FLUENT 3 March 23, 2012 14:45 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07 Dan Moskal Main CFD Forum 0 October 24, 2002 22:02

All times are GMT -4. The time now is 01:52.